[Gioacchino La Rochelle]

Hello all,
To reduce computational costs, I decided to pass to a 2D simulation of my geometry.
It is a receiver with a single inlet (bottom) and many outlets set radially and an open side to environmental air.

My question is whether my workflow is ok (after collecting infos on the web):
1. geometry obtained by revolution of a plane (about 3°)
2. mesh of 1 element depth (and for not sweepable bodies?)
3. setting interface 'rotational periodicity' on the symmetry planes?

Thanks

[ghorrocks]

1. Yes, a 3° arc is in the normal range.
2. Yes, the mesh should be 1 element thick. I do not understand the comment about sweepable bodies.
3. Normally you would put symmetry planes on both faces. You can put rotational periodicity - this will allow a velocity normal to the faces and will allow you to model swirling flows.

[Gioacchino La Rochelle]

Originally Posted by ghorrocks

1. Yes, a 3° arc is in the normal range.
2. Yes, the mesh should be 1 element thick. I do not understand the comment about sweepable bodies.
3. Normally you would put symmetry planes on both faces. You can put rotational periodicity - this will allow a velocity normal to the faces and will allow you to model swirling flows.

Thank you for the answer!
The problem I have on mesh (I haven't fixed it yet) is that even though I apply sweep method on my mesh and set 1 division, it happens that more than 1 division realises actually.

The deficit of swepable bodies is in CFX-pre, because of the setting of boundary conditions and the large number of interfaces/connectivity to set.
Is there any way to glue the mesh still in the ANSYS mesher so that I can read only outer face on CFX-pre?
I'm a bit warried about too much setting on interfaces on CFX-pre ...

[ghorrocks]

The problem I have on mesh (I haven't fixed it yet) is that even though I apply sweep method on my mesh and set 1 division, it happens that more than 1 division realises actually.

Things like this is exactly why I don't like ANSYS Meshing. You will find you have much better control over the mesh with ICEM, but it will require some effort to learn. If you want to stick with ANSYS Mesh there are ways to get it to give you the mesh you want but it is always frustrating finding it.

In DesignModeller, if you define the large number of bodies as a multi-body part then they will be meshed with a contiguous mesh and there is no need for interfaces.

[Gioacchino La Rochelle]

I succeded!
I write a little guide below.

Guide 'How to mesh any 2D domain single-body with topological issue (e.g. no sweepable bodies) using the Sweep method and local refinement without compromise mesh quality and aspect ratio'
1. Spaceclaim: build your mesh starting from a 2D sketch and pull along a rotation axis (this will reduce the error of face size) of an angle below 3°
2. ANSYS mesher: set 'Uniform' size function in global mesh setting. Set the element size and max element size as you wish according to your geometry pattern.
3. Right click on 'mesh' and add method>sweep>manual selection of source and target face. Now select the two faces of axisymmetric domain. Remember to set the number of division equal to 1.
4. Right click on 'mesh' and add 'Match control'. Select the same faces as High/Low and express the rotation axis.
5. Mesh refinement: use sphere of influence (preferred for cavity or closed volumes) or edge sizing (warning to the characteristic length of the side your considering).

Using the manual sweep setting together with the sphere of influence one can build a mesh for profile don't recognised sweepable and with aspect ratio below 20 for a domain of 24x24 m^2.